Forums

Diode (LED) parameters in LTSpice

Started by John S February 7, 2018
This is the model I'm using:

.model LXHL-BW02 D(Is=4.5e-20 Rs=.85 N=2.6 Cjo=1.18n Xti=200 Iave=400mA 
Vpk=5 mfg=Lumileds type=LED)

It is the closest selection of Vf to the diode I'm going to use. However 
it is a bit higher than the spec sheet.

How do I adjust the parameters above to get a lower Vf?

Thanks, Guys.

JohnS
>"John S" wrote in message news:p5fgb7$cc3$1@dont-email.me...
>This is the model I'm using:
>.model LXHL-BW02 D(Is=4.5e-20 Rs=.85 N=2.6 Cjo=1.18n Xti=200 Iave=400mA >Vpk=5 mfg=Lumileds type=LED)
>It is the closest selection of Vf to the diode I'm going to use. However it >is a bit higher than the spec sheet.
>How do I adjust the parameters above to get a lower Vf?
>Thanks, Guys.
IS and N. "IS" is the reverse leakage current, and nominally sets the VF for normal diodes when its its usual N= 1. For LEDS, N is set higher to get its higher VF without messing with its IS. I'm reckon here, that for this device, you need to change N to get a better match. an IS=4.5e-20 is actually a tad small for a discrete diode though. That's more of a value for a um IC diode. A discrete might weigh in at say, 10n-0.01n or larger even if a power diode. Ohh.... and what's with this "in LTSpice" shit... diode models are generic to any Spice :-) -- Kevin Aylward http://www.anasoft.co.uk - SuperSpice http://www.kevinaylward.co.uk/ee/index.html
On Wed, 7 Feb 2018 19:45:39 -0000, "Kevin Aylward"
<kevinRemovAT@kevinaylward.co.uk> wrote:

[snip]
> >Ohh.... and what's with this "in LTSpice" shit... diode models are generic >to any Spice :-) > >
Not if you use the default settings in LTspice. Any device name that already exists in the LTspice libraries becomes an idealized behavioral model... take note of the diode "parameters" you set... there ain't no "VF" parameter in a true Spice diode model. You can get around this "in LTspice" shit by supplying your own libraries AND setting SOLVER=ALTERNATE. In some ways LTspice is a good thing... it convinces "pretend" designers that they know what they are doing... they go down in flames... the boss is NOT impressed... consultants are hired... Oh! The joy !>:-} ...Jim Thompson -- | James E.Thompson | mens | | Analog Innovations | et | | Analog/Mixed-Signal ASIC's and Discrete Systems | manus | | STV, Queen Creek, AZ 85142 Skype: skypeanalog | | | Voice:(480)460-2350 Fax: Available upon request | Brass Rat | | E-mail Icon at http://www.analog-innovations.com | 1962 | It's what you learn, after you know it all, that counts.
On Wed, 07 Feb 2018 13:08:35 -0700, Jim Thompson
<To-Email-Use-The-Envelope-Icon@On-My-Web-Site.com> wrote:

>On Wed, 7 Feb 2018 19:45:39 -0000, "Kevin Aylward" ><kevinRemovAT@kevinaylward.co.uk> wrote: > >[snip] >> >>Ohh.... and what's with this "in LTSpice" shit... diode models are generic >>to any Spice :-) >> >> > >Not if you use the default settings in LTspice. Any device name that >already exists in the LTspice libraries becomes an idealized >behavioral model... take note of the diode "parameters" you set... >there ain't no "VF" parameter in a true Spice diode model. > >You can get around this "in LTspice" shit by supplying your own >libraries AND setting SOLVER=ALTERNATE. > >In some ways LTspice is a good thing... it convinces "pretend" >designers that they know what they are doing... they go down in >flames... the boss is NOT impressed... consultants are hired... Oh! >The joy !>:-} > > ...Jim Thompson
Here is an example of a SPICE model for a diode: .MODEL DFWD D + IS=17.26627E-12 + N=1.88563 + RS=21.99482E-3 + IKF=0.999979 + CJO=117.72E-12 + M=.25488 + VJ=.53537 + ISR=66.24368E-6 + NR=2.63527 + BV=330.0845 + IBV=.25878 + TT=216.40E-9 Funny, I don't see any parameters named "Iave", "Vpk" or "type"... because they're fictions of Mikey's narcissistic LTspice. Not that one can't create a reasonable model for an LED using standard Berkeley Spice diode model parameters... you can easily... just takes some real-engineering/curve-fitting thought. (I find it necessary to twiddle "EG" as well to get the TC correctly.) ...Jim Thompson -- | James E.Thompson | mens | | Analog Innovations | et | | Analog/Mixed-Signal ASIC's and Discrete Systems | manus | | STV, Queen Creek, AZ 85142 Skype: skypeanalog | | | Voice:(480)460-2350 Fax: Available upon request | Brass Rat | | E-mail Icon at http://www.analog-innovations.com | 1962 | It's what you learn, after you know it all, that counts.